Electronics > Beginners
Review 2 layer Digital only PCB design in KiCad 5.1
Kasper:
Vcc trace: make Vcc wider and try to have star layout instead of all Vcc in series.
Decoupling caps: it is best to have decoupling cap between Vcc and IC. Remove trace between pin 18 and 4 of the IC. Assuming the 10 pin connector is power input; connect Vcc from 10 pin connector through decoupling cap then into IC pin 18.
Ground pours: probably doesnt matter for this but for good practice for high frequency and emc compliance, each piece of ground should have atleast 2 vias or should be removed. Each piece should have vias near each corner. Like stitching down a piece of fabric, dont leave any corners unstitched to flap around. In other words don't leave peninsulas or else they can act as antennas.
Kasper:
Add mounting holes and test points if you think you might want them.
Silkscreen labels to the headers and test points can be handy.
Run DRC (design rules check) it should catch things like the unconnected net 'CON' near the south east corner.
Kasper:
The rings on your vias look a little thin. Drill holes sometimes dont go exactly where you want. If the ring is not much bigger than the hole and the drill is a little off then it can cut the connection between track and via. Think of the ring as the tolerance you are giving to the drill bit.
If you have space for extra tolerance, larger via holes and larger rings, use it. Not only is it easier and less risk for manufacturer, larger vias makes it easier for you to add wires to your board if you need to do mods or add test leads later.
It is good to have as few different drill sizes as possible. That means less drill bit changes for manufacturer.
lukasz.kostka:
Ok. What about now ?
I do not want to change VCC to be wider since it is impossible to route it between pins.
I've enlarged via pads.
Can't figure out a way for pin 4 VCC on atmega to go to a star point. IMO it is good enough since there will be little current.
Twoflower:
--- Quote from: Kasper on October 16, 2019, 05:50:51 am ---Decoupling caps: it is best to have decoupling cap between Vcc and IC. Remove trace between pin 18 and 4 of the IC. Assuming the 10 pin connector is power input; connect Vcc from 10 pin connector through decoupling cap then into IC pin 18.
--- End quote ---
Why? The solution now is that both VCC pins might have a reasonable big voltage difference between both VCC pins. Yes a split power plane isn't the best, but I think much better than routing the supply all over the place and open a big loop to catch up lots of noise. And there are no traces/signals crossing the area that could be affected.
If you want to prevent the ground-plane split you can rout the VCC trace close to the solder pads; preferably on the left side around.
The VCC for the upper connector: Route the signal from pin 2 to pin 15 on the back-side. If you do this, you might be able to stay on top layer with the SS signal. You can easily split the VCC above pin 5 to make space. This seems to be a digital circuit. So a strict star routing isn't necessary.
If you want to keep the VCC at the lower side of the PCB: You should remove the long finger on top-layer between the VCC and SS. Such traces might act as antennae. At least do some ground-stitching there.
An no one forbids you to use two or more trace-widths on one trace. But if the current on the traces is not that high that's probably OK as it is.
Navigation
[0] Message Index
[#] Next page
[*] Previous page
Go to full version